[blockMesh] #codeStream loop inside a blockMeshDict

francois · April 11, 2015, 12:08

Hi all,

I would like to use #codeStream to define the points of splines in a blockMeshDict.

Here is the code snippet I use:

Code:

 spline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$L/(nbPoints-1);
       scalar yi = $Ri - ($Re-$Ri) * (6*pow(xi/$L,5) - 15*pow(xi/$L,4) + 10*pow(xi/$L,3));
        os  << point(xi, -yi, 0) << endl;
        // Info  << point(xi, -yi, 0) << endl;
     }
   #};
  };
   )

The full blockMeshDict file is attached in this post.

I've got this error message:

Code:

--> FOAM FATAL IO ERROR: 
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 79 the punctuation token ';'

file: /home/beaubert/OpenFOAM/beaubert-2.3.0/run/convergentMarie/convergentCase/constant/polyMesh/blockMeshDict.edges at line 79.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 94.

FOAM exiting

The mesh is fine if I directly put the points coordinates (retrieved with Info) into the blockMeshDict.

Any idea ?
Thanks a lot for your help

Happy foaming

François

hk318i · April 15, 2015, 07:18

Just remove the red semicolon

Quote:

Originally Posted by francois

Hi all,

I would like to use #codeStream to define the points of splines in a blockMeshDict.

Here is the code snippet I use:

Code:

 spline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$L/(nbPoints-1);
       scalar yi = $Ri - ($Re-$Ri) * (6*pow(xi/$L,5) - 15*pow(xi/$L,4) + 10*pow(xi/$L,3));
        os  << point(xi, -yi, 0) << endl;
        // Info  << point(xi, -yi, 0) << endl;
     }
   #};
  };
   )

The full blockMeshDict file is attached in this post.

I've got this error message:

Code:

--> FOAM FATAL IO ERROR: 
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 79 the punctuation token ';'

file: /home/beaubert/OpenFOAM/beaubert-2.3.0/run/convergentMarie/convergentCase/constant/polyMesh/blockMeshDict.edges at line 79.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 94.

FOAM exiting

The mesh is fine if I directly put the points coordinates (retrieved with Info) into the blockMeshDict.

Any idea ?
Thanks a lot for your help

Happy foaming

François

francois · April 17, 2015, 08:36

Thank you very much hk318i !

Note for myself: always read twice before posting, especially if it's in front of my nose

Here is a working example if someone wants to try this #codeStream feature:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

// Geometry parameters

D 44.45; // Pipe diameter
Lc 263.36625; // Length of the contraction
Re #calc "$D/2.0"; // Exit radius
Ri 67.230625; // Inlet radius
H #calc "0.1*$D"; // Depth
Lp 200; // Length of the pipe
Ld #calc "$Lc+$Lp";

// Mesh parameters

Nx 20;
Ny 20;
Nz 1;

Gx 0.5;
Gy 1;
Gz 1;

// Vertices of the geometry

vertices
(

 (0  #calc "-$Ri" 0)   // Point 0
 ($Lc #calc "-$Re" 0)  // Point 1
 ($Lc $Re 0)           // Point 2
 (0  $Ri 0)            // Point 3

 (0  #calc "-$Ri" $H)  // Point 4
 ($Lc #calc "-$Re" $H) // Point 5
 ($Lc $Re $H)          // Point 6
 (0  $Ri $H)           // Point 7

 ($Ld #calc "-$Re" 0)   // Point 8
 ($Ld $Re 0)            // Point 9
 ($Ld #calc "-$Re" $H)  // Point 10
 ($Ld $Re $H)           // Point 11

);

// Blocks definition

blocks
(
 hex (0 1 2 3 4 5 6 7) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
 hex (1 8 9 2 5 10 11 6) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
);

edges
(

 BSpline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, 0) << endl;
       Info  << point(xi, -yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 4 5 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, $H) << endl;
       Info  << point(xi, -yi, $H) << endl;
     }
   #};
  }
   )

 BSpline 3 2 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, 0) << endl;
       Info  << point(xi, yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 7 6 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re-$Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, $H) << endl;
       Info  << point(xi, yi, $H) << endl;
     }
   #};
  }
   )
);

// Boundaries

boundary
(
 inlet
 {
   type patch;
   faces
     (
      (0 4 7 3)
      );
 }
 outlet
 {
   type patch;
   faces
     (
      (8 10 11 9)
      );
 }
 upperWallUpstream
 {
   type wall;
   faces
     (
      (3 2 6 7)
      );
 }
 lowerWallUpstream
 {
   type wall;
   faces
     (
      (0 1 5 4)
      );
 }
 upperWallDownstream
 {
   type wall;
   faces
     (
      (2 9 11 6)
      );
 }
 lowerWallDownstream
 {
   type wall;
   faces
     (
      (1 8 10 5)
      );
 }
 frontAndBack
 {
   type empty;
   faces
     (
      (0 1 2 3)
      (4 5 6 7)
      (1 8 9 2)
      (5 10 11 6)
      );
 }
 );

mergePatchPairs
(
);

And the result is attached below

hk318i · April 17, 2015, 09:44

Don't worry, it happens with every foamer

I have only one comment about your code, which could be useful for someone else in the future. Instead of repeating the code for each edge, you can use the codeStream directly inside edges.

Code:

edges (#codeStream { 
   code
   #{
        Calculate all the points....;
       Then
          os << "edgetype1 A B" << pointsList ;
          os << "edgetype2 A B" << pointsList ;
 
   #}
}
);

or you can define new function in separate file myfun.H and include it the you call the function in codeStream.

Code:

#codeStream
{
     codeInclude
    #{
        #include "pointField.H"
        #include "myfun.H"
    #};
            codeOptions
            #{
                -I$(FOAM_CASE)/constant/polyMesh        <-- location of myfun.H
            #};
            codeLibs
            #{

            #};
     code
    #{
          type y = myfunName(inputs);
   os <<  ........ ;
     #}

myfun.H

Code:

using namespace Foam;
type myfunName(type inputs)
{

   forAll(y, i)
   {
       y[i] = function;
   }

   return y;

}

Hopefully these tips will be useful for someone coming directly from google search.

Best wishes,
Hassan

Quote:

Originally Posted by francois

Thank you very much hk318i !

Note for myself: always read twice before posting, especially if it's in front of my nose

Here is a working example if someone wants to try this #codeStream feature:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

// Geometry parameters

D 44.45; // Pipe diameter
Lc 263.36625; // Length of the contraction
Re #calc "$D/2.0"; // Exit radius
Ri 67.230625; // Inlet radius
H #calc "0.1*$D"; // Depth
Lp 200; // Length of the pipe
Ld #calc "$Lc+$Lp";

// Mesh parameters

Nx 20;
Ny 20;
Nz 1;

Gx 0.5;
Gy 1;
Gz 1;

// Vertices of the geometry

vertices
(

 (0  #calc "-$Ri" 0)   // Point 0
 ($Lc #calc "-$Re" 0)  // Point 1
 ($Lc $Re 0)           // Point 2
 (0  $Ri 0)            // Point 3

 (0  #calc "-$Ri" $H)  // Point 4
 ($Lc #calc "-$Re" $H) // Point 5
 ($Lc $Re $H)          // Point 6
 (0  $Ri $H)           // Point 7

 ($Ld #calc "-$Re" 0)   // Point 8
 ($Ld $Re 0)            // Point 9
 ($Ld #calc "-$Re" $H)  // Point 10
 ($Ld $Re $H)           // Point 11

);

// Blocks definition

blocks
(
 hex (0 1 2 3 4 5 6 7) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
 hex (1 8 9 2 5 10 11 6) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
);

edges
(

 BSpline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, 0) << endl;
       Info  << point(xi, -yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 4 5 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, $H) << endl;
       Info  << point(xi, -yi, $H) << endl;
     }
   #};
  }
   )

 BSpline 3 2 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, 0) << endl;
       Info  << point(xi, yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 7 6 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re-$Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, $H) << endl;
       Info  << point(xi, yi, $H) << endl;
     }
   #};
  }
   )
);

// Boundaries

boundary
(
 inlet
 {
   type patch;
   faces
     (
      (0 4 7 3)
      );
 }
 outlet
 {
   type patch;
   faces
     (
      (8 10 11 9)
      );
 }
 upperWallUpstream
 {
   type wall;
   faces
     (
      (3 2 6 7)
      );
 }
 lowerWallUpstream
 {
   type wall;
   faces
     (
      (0 1 5 4)
      );
 }
 upperWallDownstream
 {
   type wall;
   faces
     (
      (2 9 11 6)
      );
 }
 lowerWallDownstream
 {
   type wall;
   faces
     (
      (1 8 10 5)
      );
 }
 frontAndBack
 {
   type empty;
   faces
     (
      (0 1 2 3)
      (4 5 6 7)
      (1 8 9 2)
      (5 10 11 6)
      );
 }
 );

mergePatchPairs
(
);

And the result is attached below

francois · April 17, 2015, 10:03

Thanks Hassan for your kind and very relevant suggestions.

I was thinking myself of refactoring the code which was submitted here only as proof of concept for myself or other newcomers to #codeStream.

Anyway, those are indeed very nice additions to put into the code, thanks !
I may put all this stuff on the wiki when I'll find the time.

You're a good example that illustrates why I like so much the OpenFOAM community.
Happy foaming

hk318i · April 29, 2015, 13:25

Hello!
I hit one of the codeStream limitations today. I would like to share it with everyone here.

Code:

string "
         int N = 100;
         scalar cw = $cw*$ftTom; // chord
         scalar..."
    is too long (max. 8000 characters)

Although I used the method which I mentioned above, I had to write a very very long codeStream. Fortunately, I found a solution for this problem which is dividing the code stream to many .H files and includes directly inside the code not as a header file.

Code:

    code
    #{
#include "myLongCode.H"
     #};

BUT, there is a drawback for this method, you cannot use the macro substitutions ($parameter). I desperately tried "#inputMode merge" but it doesn't work.
So to read any variable from the blockMeshDict in this case, you have to lookup it.

Code:

scalar a = readScalar(dict.lookup("a"));

Next time, I have to FOAM responsibly

arieljeds · October 1, 2015, 07:07

On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

hk318i · October 1, 2015, 09:09

Quote:

Originally Posted by arieljeds

On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

You can use

Code:

paraFoam -block

It shows the points so you could create the blocks which is really helpful.
I am not sure if that what you are looking for or not. Maybe you mean if you have list called points and you want use points[5] in blocks.
In this case, based on my experience, you cannot do that directly because the variables are limited to codeStream scope.

BUT there is a way around this problem which is including the blocks section inside the same codeStream as points. Then use os stream to print blocks as well. Or you can write a script (using python or octave or m4 .) to create blockMesh file.

arieljeds · October 1, 2015, 09:18

Hi there,

Thanks for that. Actually I wasn't sure if that would work without running blockMesh first...

Ok just tried and how is it possible to do this without first building the blocks? Or do I just put:

Code:

blocks
(
);

And leave the blocks blank?

hk318i · October 1, 2015, 09:26

It works without executing blockMesh, just make sure that boundary is empty as well. It will show you the points and edges

arieljeds · October 1, 2015, 09:28

perfect! Thanks for that... very difficult to find something so simple online!

arieljeds · October 1, 2015, 09:55

Sorry, last question.. say I'm trying to duplicate both the z points (as done in the cylinder tutorial) and the y points. I tried to just include a second loop as follows:

Code:

label sy = points.size();
points.setSize(2*sy);
for (label i = 0; i < sy; i++)
{
     const point& pt = points[i];
     points[i+sy] = point(pt.x(), -pt.y(), pt.z());
}

os << points;

But this (perhaps obviously) didn't work... Can you offer any guidance on the correct syntax to use?

hk318i · October 2, 2015, 03:26

What is pt? This expression looks wrong.

arieljeds · October 2, 2015, 05:23

I took that directly from the cylinder tutorial (uses potentialFoam) but I believe pt the name of the pointer that points to the location of that point?

hk318i · October 2, 2015, 05:36

Sorry, I did see the first expression in the loop. The code should work without errors.

arieljeds · October 2, 2015, 05:38

The code works without errors when I have the second loop to duplicate the y-values but it doesn't actually duplicate the y-values. It does duplicate the z-values successfully but I'm not sure why it isnt' fully working to duplicate everything. Any thoughts?

hk318i · October 2, 2015, 05:41

Try to print the points to see the values.

Code:

Info << points << endl;

ninoleum · October 22, 2015, 15:43

Hi all,
taking inspiration from this thread, I tried to generate my geometry with #codestream directive inside blockMeshDict (the method is really smart indeed and overcomes the difficulty of "manual meshing - the trappist way

" with plain text blockMeshDict, so thanks Francois and Hassan for sharing this conversation!).
The mesh I obtain is apparently correct but if I run checkMesh against it, the situation is much different:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : checkMesh -constant
Date   : Oct 22 2015
Time   : 21:18:35
Host   : "rocchigi1npge"
PID    : 2009
Case   : /home1/rok/Cases/helix
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = constant

Time = constant

Mesh stats
    points:           63529
    faces:            178576
    internal faces:   167024
    cells:            57600
    faces per cell:   6
    boundary patches: 1
    point zones:      0
    face zones:       0
    cell zones:       2

Overall number of cells of each type:
    hexahedra:     57600
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    defaultFaces        11552    11554    ok (closed singly connected)      

Checking geometry...
    Overall domain bounding box (-0.07529996 -0.008 -0.07529993) (0.07529996 0 0.0753)
    Mesh (non-empty, non-wedge) directions (0 0 0)
    Mesh (non-empty) directions (0 0 0)
 ***Number of edges not aligned with or perpendicular to non-empty directions: 122876
  <<Writing 63529 points on non-aligned edges to set nonAlignedEdges
    Boundary openness (-4.773914e-18 -8.73355e-16 6.456257e-18) OK.
    Max cell openness = 3.404553e-16 OK.
    Max aspect ratio = -1 OK.
    Minimum face area = 1.547883e-08. Maximum face area = 1.802198e-05.  Face area magnitudes OK.
 ***Zero or negative cell volume detected.  Minimum negative volume: -5.256213e-09, Number of negative volume cells: 57600
  <<Writing 57600 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 180 average: 178.9199
 ***Number of non-orthogonality errors: 167024.
  <<Writing 167024 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 345600 faces are incorrectly oriented.
  <<Writing 178576 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 0.1232568 OK.
    Coupled point location match (average 0) OK.

Failed 4 mesh checks.

End

Please note that checkMesh complains about the negative volume for each and every one of the 57600 cells which compose the mesh and about the non-orthogonality of each and every of the 167024 internal faces.
I checked several time the definition of each block for the vertexes sequence without finding any error.
I attached here the blockMeshDict for your reference.
So: what I am doing wrong?

Thank You

Gianluca

wyldckat · October 22, 2015, 15:49

Quick answer: Negative volume is usually related to the vertices being order in the wrong direction.

hk318i · October 23, 2015, 07:12

I totally agree with Bruno, most probably one there is a block is not following the right had rule.

I tried to run your code using OpenFOAM2.3.x and I got few errors. I don't know if you are facing the same errors or not. I had to modify minor things to run it. I tested it also on OpenFOAM-dev hoping that the new updates will overcome your problem but unfortunately not. The new updates are related to boundary definition only.

I attached the modified file here in case you needed it. I just modified the x and y type to scalarField. Also changed the int to label (which is exactly the same (just a habit)).

Best Wishes
Hassan

April 17, 2015, 10:03		#5
francois Senior Member Francois Beaubert Join Date: Mar 2009 Location: Lille, France Posts: 147 Rep Power: 17	Thanks Hassan for your kind and very relevant suggestions. I was thinking myself of refactoring the code which was submitted here only as proof of concept for myself or other newcomers to #codeStream. Anyway, those are indeed very nice additions to put into the code, thanks ! I may put all this stuff on the wiki when I'll find the time. You're a good example that illustrates why I like so much the OpenFOAM community. Happy foaming hk318i likes this.

April 29, 2015, 13:25		#6
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	Hello! I hit one of the codeStream limitations today. I would like to share it with everyone here. Code: string " int N = 100; scalar cw = $cw*$ftTom; // chord scalar..." is too long (max. 8000 characters) Although I used the method which I mentioned above, I had to write a very very long codeStream. Fortunately, I found a solution for this problem which is dividing the code stream to many .H files and includes directly inside the code not as a header file. Code: code #{ #include "myLongCode.H" #}; BUT, there is a drawback for this method, you cannot use the macro substitutions ($parameter). I desperately tried "#inputMode merge" but it doesn't work. So to read any variable from the blockMeshDict in this case, you have to lookup it. Code: scalar a = readScalar(dict.lookup("a")); Next time, I have to FOAM responsibly

October 1, 2015, 09:18		#9
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi there, Thanks for that. Actually I wasn't sure if that would work without running blockMesh first... Ok just tried and how is it possible to do this without first building the blocks? Or do I just put: Code: blocks ( ); And leave the blocks blank?

October 1, 2015, 09:55		#12
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Sorry, last question.. say I'm trying to duplicate both the z points (as done in the cylinder tutorial) and the y points. I tried to just include a second loop as follows: Code: label sy = points.size(); points.setSize(2*sy); for (label i = 0; i < sy; i++) { const point& pt = points[i]; points[i+sy] = point(pt.x(), -pt.y(), pt.z()); } os << points; But this (perhaps obviously) didn't work... Can you offer any guidance on the correct syntax to use?

October 2, 2015, 03:26		#13
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	What is pt? This expression looks wrong. __________________ @HIKassem \| HassanKassem.me

October 1, 2015, 07:07		#7
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

October 1, 2015, 09:26		#10
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	It works without executing blockMesh, just make sure that boundary is empty as well. It will show you the points and edges

October 1, 2015, 09:28		#11
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	perfect! Thanks for that... very difficult to find something so simple online!

October 2, 2015, 05:23		#14
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	I took that directly from the cylinder tutorial (uses potentialFoam) but I believe pt the name of the pointer that points to the location of that point?

October 2, 2015, 05:36		#15
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	Sorry, I did see the first expression in the loop. The code should work without errors.

October 2, 2015, 05:38		#16
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	The code works without errors when I have the second loop to duplicate the y-values but it doesn't actually duplicate the y-values. It does duplicate the z-values successfully but I'm not sure why it isnt' fully working to duplicate everything. Any thoughts?

October 2, 2015, 05:41		#17
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	Try to print the points to see the values. Code: Info << points << endl;

October 22, 2015, 15:49		#19
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,975 Blog Entries: 45 Rep Power: 128	Quick answer: Negative volume is usually related to the vertices being order in the wrong direction. hk318i, ninoleum and kooki_13 like this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field	lakeat	OpenFOAM Community Contributions	58	December 23, 2021 02:36
[Other] refineWallLayer Error	Yuby	OpenFOAM Meshing & Mesh Conversion	2	November 11, 2021 11:04
Star-CCM+ Macro - Loop over just wall boundary conditions	jbatchel	STAR-CCM+	5	March 2, 2018 13:42
Pressure distribution on a wall	darazsbence	CFX	17	October 6, 2015 10:38
How to determine a point is inside a tetrahedral?	G.P. Xia	Main CFD Forum	16	January 12, 2000 11:15